Need Help!- 6T-B control and G50... How to set?

[grweldon]

I'm a quite seasoned operator/programmer but at 49 years old, the 6T control was a bit before my time as an operator. Now, my shop has a lathe with one of these controls and I need to know how to program it. I can understand the diagram in the manual and can see what the G50 tells the machine, but I do not know how to arrive at the correct values or how to set them.

All the Fanuc controls I have used have a "measure" feature and a geometry offset page, a tool offset page and a work coordinate page. This control only has a tool offset page.

Can anybody please post a step-by-step procedure that an engineer can follow along with to arrive at the correct values for G50 X and Z? Any and all help would certainly be appreciated...

Thanks...

[Chrliev]

G50 does 2 things, it sets the tool position relative to the part zero and also the maximum spindle speed limit for Constant Surface Speed control...

To set it properly:
Using manual jog mode, turn the OD of a part. Measure this diameter. By preset, reset or machine lock, change the machine register to display this value without moving the tool from this diameter. Do the same for Z axis, face end of part and set Z register to zero.

Move machine to safe distance, like where all tools will clear when indexing. The distance displayed will be your values for G50 line. An S code in this line would limit the maximum spindle speed to that "S" value.

G50 X5.00 Z5.00 S3500;

Tool would turn a 5" diameter and is 5" from Z zero, face , etc. Spindle will not exceed 3500 RPM good for large chucks and flimsy setups...

[grweldon]

Thank you Chrliev,

I appreciate your reply and with the additional research I've done since I made the post this morning, it makes perfect sense. I assume that if I use the home point of the machine as the "safe point" all will be well?

In other words, I take my test cuts just like I normally would on any machine that didn't have a tool probe, set my display to the measured value on X and Z, then execute a G28 U0 W0. Then the displayed values on the relative position screen (where I changed the values to match my measured values) will be the numbers that I insert in the program for the G50 X and Z...correct?

Thanks for your help...awaiting your verification...

[Chrliev]

Yes, that's correct and usually how I did it when I programmed Fanuc lathes, it works with all versions of Fanuc controlled lathes. In this way offsets are only used for small dimensional adjustments...

Charlie

[angelw]

Originally Posted by grweldon Thank you Chrliev, I appreciate your reply and with the additional research I've done since I made the post this morning, it makes perfect sense. I assume that if I use the home point of the machine as the "safe point" all will be well? In other words, I take my test cuts just like I normally would on any machine that didn't have a tool probe, set my display to the measured value on X and Z, then execute a G28 U0 W0. Then the displayed values on the relative position screen (where I changed the values to match my measured values) will be the numbers that I insert in the program for the G50 X and Z...correct? Thanks for your help...awaiting your verification...

One other thing that's important when using G50's, is the relationship between when the tool offset is applied and canceled, and when the G50 is executed.

With Geometry Offset programming, its OK to call the tool and tool offset at the same time. However, if you were to call the tool in the following way before executing the G50, then the position of the tool will be out relative to the work zeros.
This will result in a position error equal to the tool offset value.
T0101
G50 X100.000 Z200.000
G96 S200 M03
G00 X??? Z??? M08

The better method is as follows
T0100
G50 X100.000 Z200.000
G96 S200 M03
G00 X??? Z??? T0101 M08

Likewise, you should cancel the offset on the way back to the tool change position.

On long beg machines, there is often a movable Z Reference Return deceleration dog that can be set to vary the Z Reference Return position. In this way, time is not being wasted going a long way back to a Z Zero position for a tool change if the workpiece is quite short. However, on machines that don't have this feature, the following program format is useful and employs long and short G50s

N1 G21 G40
G50 T0100 S2000
G50 X150.00 Z150.000
/G28 U0.0 W0.0
/G50 X400.000 Z500.000
G00 X??? Z??? T0101 M08
.........
.........
.........
G00 X200.000 Z200.000 T0100 M09
/G50 X400.000 Z500.000
M01
(NEXT TOOL)
N2 G50 T0200 S2500
G50 X150.00 Z150.000
/G28 U0.0 W0.0
/G50 X350.000 Z450.000
G00 X??? Z??? T0202 M08
.........
.........
.........
G00 X125.000 Z250.000 T0200 M09
/G50 X350.000 Z450.000
M01
(NEXT TOOL)
etc

G50s at the Reference Return position are easiest to obtain because of the fixed reference point. Once you have these, the relative difference between the various tool G50s can be compared and G50s for a short tool change position calculated as in the above example. The above method proves to be quite fool proof, in that if you have to stop the machine for any reason, just turn the block delete switch off, make sure the tool is clear of the work, place the cursor at the start of the the code for that tool and press the cycle start button. The Short G50 will be read, then because the block delete is off, the tool will return to the Reference Return position, read the Long G50 and execute the following blocks without disaster. Once the tool is past the block deleted code, the block delete switch can be turned on again so that the program again operates from the Short G50 tool change position.

The above is not so important on a low volume, or one off job, but can eat some time if the number was substantial and the program is operating from the Reference Return position.

Regards,

Bill

[grweldon]

Thank you Bill, I appreciate the detailed response. I think I can handle the G50 programming... now if I could only figure out how to enter MDI commands into the ancient Fanuc 6T!

[angelw]

Originally Posted by grweldon Thank you Bill, I appreciate the detailed response. I think I can handle the G50 programming... now if I could only figure out how to enter MDI commands into the ancient Fanuc 6T!

1. Select MDI mode via the mode selection switch.
2. Press the Program button.
3. Press the Page Down button repeatedly until the MDI page is displayed
4. Use the key pad to write the desired code One Word at a time
5. Press the Input button to register each word into memory.
6. Input EOB to finish.
7. Press Input Start, or Cycle Start to execute the command. This will depend on how the machine has been set up. Some machines used Input Start, others used the Cycle Start button.

Regards,

Bill

[bertus.nl]

i only use the g50 with the max spindel speed.
never with x or z, for it does increment movement .
so when you interupt youre program and jump into youre program on a different position you get the chance that you crash.
if you want to go to a safe tool chance point,just type :
G0 G90 X300 Z200 ABSOLUTE is always safe!!!

vr gr bertus.nl

[angelw]

Originally Posted by bertus.nl i only use the g50 with the max spindel speed. never with x or z, for it does increment movement . so when you interupt youre program and jump into youre program on a different position you get the chance that you crash. if you want to go to a safe tool chance point,just type : G0 G90 X300 Z200 ABSOLUTE is always safe!!! vr gr bertus.nl

You don't specify the control you're using, but the OP was related to a Fanuc 6T-B. Incremental moves with this control are specified with U and W for the respective absolute addresses X and Z; G90 is the absolute command for a mill control and specifies a Cutting Cycle command for the 6T control.

To be able to go to a safe tool change position specified by an absolute command such as X300 Z300, a coordinate system must be set so that the control knows where that absolute position is. That's what G50 in association with X and Z, in a control that does not have Geometry Offset Programming and Work Shift offsets, is used for.

Regards,

Bill